User Guide V10 SP1 Addendum

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1 Alibre Design User Guide V10 SP1 Addendum

2 Copyrights Information in this document is subject to change without notice. The software described in this document is furnished under a license agreement or nondisclosure agreement. The software may be used or copied only in accordance with the terms of those agreements. No part of this publication may be reproduced, stored in a retrieval system, or transmitted in any form or any means electronic or mechanical, including photocopying and recording for any purpose other than the purchaser s personal use without the written permission of Alibre, Inc. Alibre, Inc Campbell Creek Blvd. Suite 100 Richardson, TX USA Alibre, Inc. All rights reserved. Alibre and the Alibre logo are registered trademarks; Alibre Design and Alibre PhotoRender are trademarks of Alibre Inc. in the United States and/or other countries.

3 Contents Drawings Creating a New Drawing Selecting a Drawing Template Inserting Standard Views Saving and Opening a Drawing Working in a Drawing Updating Drawing Views Reordering Sheets Dimensioning Inserting Additional Views Detail View Section View Partial View Exploded View Custom Templates Annotations Note Datums Datum Targets Feature Control Frames Surface Finish Symbol Weld Symbol Editing and Deleting Annotations...28 i

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5 C HAPTER 12 Drawings This User Guide Addendum contains updated information for SP1 in various sections of chapter 12 of the Alibre Design v10 User Guide Creating a New Drawing Selecting a Drawing Template You can select from a number of standard drawing templates, your own custom templates, or a blank drawing of varying size. ANSI, DIN, and ISO drawing templates are supported. To select a drawing template: 1. In the New Sheet Properties dialog, select Template or Blank Sheet. 2. If you selected Template, also select a standard drawing template from the list. To use a custom drawing template not listed, click Browse and select the template from the Custom Drawing Template dialog. OR, if you selected Blank Sheet, select a sheet size from the list. Note: If you have previously browsed to another template folder, you can use the Default button to reset the template list back to the system template folder. 3. If desired, enter a name for the sheet in the Sheet Name field. 4. In the Default View Scale area, specify the scale to use in the drawing. The scale can be changed later if necessary. 5. To create a drawing with no models associated with it, check the Create An Empty Drawing box. 6. Click OK. If you selected a standard or custom template, the Fill In Text dialog may appear. 1

6 Inserting Standard Views You can select which standard views you initially want to create in the drawing. You can insert additional standard views later as necessary. To insert the standard views: 1. A preview of the selected part or assembly is shown in the Front View preview window. To select a different part, click the Browse button to make a new selection. 2. Select the view that you want to use as the Front View in the drawing. You can use the arrow buttons to reorient the view in the preview window. You can also click the Workspace Orientation button to select from default and custom views created in the part or assembly workspace. 2

7 3. In the View Selections area select the views that you want to insert into the drawing. The default views are Front, Top, and Right. To add or remove a view, click the view's corresponding button. 4. If multiple configurations of the design exist, select which one you want to use for these views from the Configurations list. 5. In the case of assemblies, if any exploded views were created in the assembly workspace, you can also select an exploded view from the Exploded Views list. 6. To see all of the options at the bottom of the dialog, if they are not visible, click the More Options button. 7. In the View Creation Options section: a. Check the Fast Views box to use Fast View Mode on these views. Fast View mode produces a less precise image (visually), but is substantially faster for large or very complex assemblies. b. Enter a value for the view scale into the Scale field; or, check the option Use Sheet scale, which will select the Sheet scale that was set in the New Sheet Properties dialog. c. Select the Project as Flat Pattern option if desired for sheet metal parts. 8. In the View Detailing Options section: a. Check Select All to enable all of the available options. b. Check Hidden Lines to display the entities that would not be directly visible. c. Check Centermarks and/or Centerlines if you want to display them. 3

8 d. Check the Design Dimensions box if you want to display the driving dimensions from the model. (These will be the original model dimensions. If you have used any Push/Pull functions, the final model dimensions resulting from those will not be displayed.) e. Check Hole Callouts to display the full hole callout for holes created using the Hole feature. f. Check Cosmetic Threads to display a representation of the threads on a threaded hole. g. Check Tangent Edges to include the tangent edges in the view. h. Check Bend Centerlines to add center lines to bends in sheet metal parts. i. Check Part Trails to include the trail lines for exploded views of assemblies. 9. Click OK to create the views. Previews of the selected views are displayed in the work area. Note that the cursor is essentially tied to the front view. As you move the cursor, the views will all move together. 10. Move the cursor to dynamically re-position the front view to the correct location within the drawing sheet. 11. Click to place the front view. The corresponding views are also placed. The dimensions that were used to create the part are displayed automatically in the corresponding view (if you checked the option to include design dimensions). The Drawing Explorer on the left side of the work area lists the sheets associated with the drawing as well as the views associated with each sheet. The associated design is also listed under the view. 4

9 NOTE: Alibre Design supports both First Angle and Third Angle projection methods. You can set the projection method for a drawing in the Detailing tab of the Drawing Properties dialog. Click Properties in the File main menu to bring up the Drawing Properties dialog Saving and Opening a Drawing No updates to section Working in a Drawing Updating Drawing Views It is likely that you will need to make changes to your part and assembly models even after you have created 2D drawings of the models. When you make a change to a part or assembly model and save the model, the 2D drawing becomes outdated, because it does not contain the most recent model information. You can update the drawing to bring in the new model data. To update drawing views: 1. Select the Reproject Outdated Views tool from the Detailing toolbar; or, from the Tools menu, select Reproject Outdated Views. The Reproject dialog appears. 2. Choose one of the following options: a. Fast Views - the outdated items will be projected in Fast View mode b. Precise Views - the outdated items will be projected in the standard mode c. Retain View Mode - the outdated views will be projected in whichever mode they are currently in 3. Click OK to continue updating the drawing. Note: If you do not want to reproject your views, click Cancel. If you do not reproject your views, your 2D drawing will continue to be out of date, you will have limited editing options when working with your 2D Drawing until you reproject all outdated views. 5

10 Reordering Sheets You can quickly change the order of the sheets in the drawing file. To reorder the sheets: 1. Select the Reorder Sheets tool from the Detailing toolbar; or, from the Edit menu, select Reorder Sheets. The Reorder Sheets dialog appears. 2. Click the sheet you want to move. 3. Choose the appropriate button on the right to move the sheet to the desired position. 4. Click OK to accept the new sheet order and exit the dialog Dimensioning No updates to section Inserting Additional Views Detail View A detail view is a view that shows a portion of an existing view at an enlarged scale. To create a detail view: 1. Select the Activate 2D Sketch tool from the Sketching toolbar. 2. Sketch any closed figure enclosing the area that you want to detail. 6

11 3. Select the Detail View tool from the Detailing toolbar; or from the Insert menu, select Detail View. 4. Select the sketch figure. A preview of the detail view appears. 5. Move the mouse to position the detail view appropriately. The detail view can be placed anywhere on the sheet. Click to locate the view. The default scale for the detail view is the same as the sheet scale. To enlarge the detail view, right-click it and select Scale from the pop-up menu. You can place dimensions on the detail view. You can also change both the detail circle label and the detail note. To change either, double-click the text or right-click the text and select Edit from the pop-up menu. The Note dialog appears containing the original text. Enter the new text and click OK. Also, in the Detailing tab of the Drawing Properties dialog, you can pre-define the border style and font used for detail circles and detail view labels. When using a sketched circle for the detail view, the leader line and annotation positions are determined by the last location of the mouse before finalizing the circle you sketched as the reference. To change the detail location: 1. Choose the Select tool from the View toolbar if it is not already selected. 7

12 2. Move the cursor over the detail circle annotation. The annotation is highlighted and the cursor changes. 3. Click and drag the detail circle annotation to the new location. 4. Release the mouse button to reposition the circle. You will see a dialog letting you know that moving the annotation will update the dependent views. 5. Choose Yes to continue, or No to cancel the operation. If you choose Yes, the detail view is updated automatically to reflect the detail circle position change. (You can turn the prompt off if desired - from the Tools menu, select Options. On the General tab, uncheck Prompt when detail, section, or partial view annotation moved.) To change the location of detail labels: You can move both the label for the detail view, as well as the label for the detail area. 1. Click the Select tool from the View toolbar if it is not already selected. 2. Move the mouse pointer over the detail annotation. The annotation is highlighted and the mouse pointer changes. 3. Click and drag the annotation to the desired location. To change the detail area size: 1. Click the Select tool from the View toolbar if it is not already selected. 8

13 2. Move the cursor over the detail circle annotation. The annotation is highlighted and the cursor changes. 3. Double-click the annotation. The Detail View Annotation dialog appears and the circle center node is displayed. 4. Move the cursor over the circle. 5. Click and drag to resize. 6. Release the mouse button when the circle is resized appropriately. 7. Click OK in the Detail View Annotation dialog. The detail view is updated automatically to reflect the change in size of the detail area Section View A section view represents a 2D cross-section of a model. Section views are created from other views and are dependent on them. You can create a normal section view or a stepped section view. To create a normal section view: 1. Sketch a straight line across the view to define the section location. Make sure you are sketching in the view by selecting the view in the Design Explorer before entering Sketch Mode. 2. Select the Section View tool from the Detailing toolbar; or from the Insert menu select Section View. 9

14 3. Select the line that you sketched in step 1. A preview of the section view appears in the drawing. 4. Drag the section view preview to the appropriate location on the sheet. You will only be able to move the view in a direction normal to the section line. 5. Click to place the view. Notes: In the Detailing tab of the Drawing Properties dialog, you can pre-define the display style for the section line, the font for the section line label, and the default hatch pattern style. For advanced users who want to customize the available hatch patterns in Alibre Design: You can modify the predefined hatch patterns that ship with Alibre Design by editing the text file, alibre_unicode.pat. You can use Notepad to edit this file. A definition of the file format is embedded within the file. This file is located in the folder C:\Documents and Settings\All Users\Application Data\Alibre Design\System Files. To modify a section view: To edit the letter label on the section line or the note on the section view, double-click the item, or right-click and select Edit from the pop-up menu. The Note dialog appears containing the original text. Enter the new text and click OK. To change the cut direction, right-click the section view and select Reverse Section View from the pop-up menu. The section view crosshatch pattern is set in the Detailing tab on the Design Properties dialog (File > Properties). You can modify the crosshatch pattern for an individual section view. Right-click the section view and select Change Cross Hatch from the pop-up menu. The Hatch Properties dialog appears. Select a new crosshatch pattern from the list or modify the Scale or Angle. Click OK to apply the changes. 10

15 To create a stepped section view: 1. Sketch a series of line segments across the view to define the section location. 2. Select the Section View tool from the Detailing toolbar; or from the Insert menu, select Section View. 3. Select any of the line segments that you sketched in step 1. A preview of the section view appears in the drawing. 4. Drag the section view preview to the appropriate location on the sheet. You will only be able to move the view in a direction normal to the section line. 5. Click to place the view. 11

16 To redefine the section location (either normal or stepped): 1. Select the Select tool from the View toolbar if it is not already selected. 2. Move the cursor over the section line annotation. The annotation is highlighted and the cursor changes. 3. Click and drag the line to the desired location. 4. Release the mouse button to place the line. You will see a dialog letting you know that moving the annotation will update the dependent views. 5. Choose Yes to continue, or No to cancel the operation. If you choose Yes, the section view is updated automatically to reflect the section line position change. (You can turn the prompt off if desired - from the Tools menu, select Options. On the General tab, uncheck Prompt when detail, section, or partial view annotation moved.) To change the location of section view labels: You can move the label for the section view, as well as the labels for the section line. 1. Click the Select tool from the View toolbar if it is not already selected. 2. Move the mouse pointer over the annotation. The annotation is highlighted and the mouse pointer changes. 3. Click and drag the annotation to the desired location. To change the direction of the section view: 1. Right-click the section view in the work area and select Reverse Section View from the pop-up menu. Or Right-click the section view in the Drawing Explorer and select Reverse Section View from the pop-up menu. 2. The section line is flipped and the section view is displayed from the opposite direction. 12

17 To change the hatch pattern for all parts in the section view: 1. Right-click the section view in the work area and select Change Cross Hatch from the pop-up menu; or right-click the section view in the Drawing Explorer and select Change Cross Hatch from the pop-up menu. The Hatch Properties dialog appears. 2. Select a new cross hatch pattern from the Pattern pull down menu. 3. Specify the cross hatch Scale. 4. Specify the cross hatch Angle. 5. If desired, you can also modify the color, line weight, and offset distance for the hatch pattern. 6. Click OK to apply the new cross hatch pattern. Note: You can also access the cross hatch settings from the Drawing Properties dialog. From the File menu, select Properties and then select the Detailing tab in the dialog. To change the hatch pattern for individual parts in a section view: 1. In the Drawing Explorer, expand the assembly under the section view to reveal the individual parts displayed in the section. 2. Right-click the desired part and choose Change Cross Hatch from the pop-up menu. The Hatch Properties dialog appears. 3. Modify the hatch pattern properties as desired. 4. Click OK to apply the new cross hatch pattern to the selected part Partial View You can modify an existing view to create a partial view. A partial view allows you to only show a portion of an existing view. 13

18 To insert a partial view: 1. Click the Select tool from the View toolbar if it is not already selected. 2. Select the view that you wish you transform into a partial view, then select the Sketch Mode tool from the Sketching toolbar. Partial views can be created from any other view, including primary and dependent views. 3. Sketch any closed figure enclosing the area that you wish to keep in the partial view. 4. Select the Partial View tool from the Detailing toolbar; or from the Insert menu select Partial View. 5. Select the sketched closed figure. The view will transform into a partial view. 14

19 To change the partial view area size: 1. Choose the Select tool from the View toolbar if it is not already selected. 2. Move the mouse pointer over the partial view area dashed outline. 3. Right-click the dashed outline and select Edit. The Partial View Annotation dialog appears. 4. Make any necessary changes to the partial view outline. You can only modify the exiting sketch lines; you cannot sketch new ones. 5. In the Partial View Annotation dialog, select Cancel to discard the changes, or OK to update the partial view. To move the partial view area: 1. Click the Select tool from the View toolbar if it is not already selected. 2. Move the mouse pointer over the partial view area dashed outline. 3. Click and drag the outline to a new position in the view. You will see a dialog letting you know that moving the annotation will update the dependent views. 4. Choose Yes to continue, or No to cancel the operation. If you choose Yes, the partial view is updated automatically to reflect the view outline's position change. (You can turn the prompt off if desired - from the Tools menu, select Options. On the General tab, uncheck Prompt when detail, section, or partial view annotation moved.) Exploded View You can insert a 2D exploded view representation of any exploded view you created in the assembly workspace. 15

20 To create an exploded view of an assembly: 1. Select the Standard Views tool from the Detailing toolbar; or from the Insert menu, select Standard Views. The Standard Views Creation dialog appears. 2. In the Design area, select the assembly item from the drop down list that you want to insert an exploded view of; or click Browse to select the assembly from the Document Browser. Any exploded views that were saved with the assembly are subsequently listed in the Exploded Views drop down list. 3. Select the appropriate exploded view to insert. 4. Use the arrow buttons in the Front View area as well as the View Selection buttons to select the appropriate exploded view orientation(s). 5. Click OK. A preview of the exploded view appears in the work area. 6. Move the cursor to position the view. 7. Click to place the exploded view on the sheet. Note: You can toggle on and off the trail lines of an exploded view by right clicking on the view and selecting Show Part Trails Custom Templates No updates to section

21 12.7 Annotations Note You can create a free-floating note or a note with a leader pointing to an edge or face. The note can contain both text and symbols. In a part or assembly, you can attach annotations to solids. In a drawing, you can attach annotations to any view, or to the projected edge of a model. To insert a note: 1. In any workspace, from the Insert menu select Annotation > Note; or in a drawing workspace, select the Note tool from the Detailing toolbar. The Note dialog appears. 2. In the Note area, type the annotation text. You may align the text vertically and horizontally by clicking the text alignment icons above the Note field. 3. Click Font to specify the font, font style, size, color, and effects. 4. To insert a symbol, click the Symbols button. The Insert Alibre Design Symbols dialog appears. Click a symbol to insert it. Click Close to close the symbols box. 5. Specify a Rotation Angle if required. 6. If you want to include a leader, click the Show option in the Leader area. 17

22 7. Select the Bent option if you want the leader line to have a short horizontal segment near the annotation. 8. From the Arrow pull-down menu, select the arrow type you want to use. 9. From the Position pull-down menu, select the position in which the text will be placed in relation to the leader. 10. Select Smart Anchor if desired. The smart anchor option will automatically adjust the position of the text if the leader is re-positioned. The smart anchor option overrides the position selection in step Move the mouse in the work area. A preview of the annotation appears attached to the mouse pointer. Left click once to place the leader line. Left click again to place the annotation. The text appears in light blue. 12. Click Apply to accept the annotation placement (or you can double-click). The dialog remains open so you can continue to place additional annotations. Before choosing Apply, you can reposition the annotation while it is light blue in color. To do this, left click on the leader line or the text, whichever you wish to move, and release the mouse button. Move the mouse to reposition. Left click again to place it. 13. Click Close to exit the dialog. Note: You can copy and paste note annotations on the same sheet or paste them on another sheet in the same drawing file. To copy the annotation: click on it to select it (press and hold the Shift key to select multiple annotations). Then, either right click and choose Copy; or, from the Edit menu, select Copy. To paste the annotation: you can choose Paste from the Edit menu, or you can move your mouse to the location you want to paste the annotation and press CTRL + V on your keyboard Datums In a part or assembly, you can attach annotations to solids. In a drawing, you can attach annotations to any view, or to the projected edge of a model. 18

23 To insert a datum annotation: 1. In any type of workspace, from the Insert menu select Annotation > Datum. In a drawing workspace, select the Datum tool from the Detailing toolbar. The Datum Annotation dialog appears. 2. In the Datum Label box, specify the letter you wish to start the datum series with. 3. Select the Show option if want to use a leader with the datum. Select the Bent option if you want the leader line to have a short horizontal segment near the annotation. 4. From the Position pull-down menu, select the position in which the text will be placed in relation to the leader. 5. Select Smart Anchor if desired. The smart anchor option will automatically adjust the position of the text if the leader is re-positioned. The smart anchor option overrides the position selection in step From the Arrow pull-down menu, select the type of arrow to use with the leader. 7. Move the mouse in the work area. A preview of the annotation appears attached to the mouse pointer. Left click once to place the leader line. Left click again to place the annotation. The text appears in light blue. 8. Click Apply to accept the annotation placement (or you can double-click). The dialog remains open so you can continue to place additional annotations. Before choosing Apply, you can reposition the annotation while it is light blue in color. To do this, left click on the leader line or the text, whichever you wish to move, and release the mouse button. Move the mouse to reposition. Left click again to place it. 19

24 9. Click Close to exit the dialog. Datums can be resized and repositioned by clicking the text and dragging. This will change the length of the leader, as well as reposition the datum box. Datums can also be moved to another location by clicking the arrow, as opposed to the text Datum Targets In a part or assembly, you can attach annotations to solids. In a drawing, you can attach annotations to any view, or to the projected edge of a model. To insert a datum target: 1. In any type of workspace, from the Insert menu select Annotation > Datum Target. In a drawing workspace, select the Datum Target tool from the Detailing toolbar. The Datum Target Annotation dialog appears. The top area of the Datum Target dialog previews the annotation as you build it. 20

25 2. Select the target type: Point, Circular, or Rectangular. 3. In the Area fields, specify the target size. 4. Select the Show option to show or hide the datum target. 5. Select the Show size outside symbol option if desired. 6. In the Target notation fields, specify the datum reference label(s). 7. Select the Bent Leader option if necessary. 8. Move the mouse in the work area. A preview of the annotation appears attached to the mouse pointer. Left click once to place the leader line. Left click again to place the annotation. The text appears in light blue. 9. Click Apply to accept the annotation placement (or you can double-click). The dialog remains open so you can continue to place additional annotations. Before choosing Apply, you can reposition the annotation while it is light blue in color. To do this, left click on the leader line or the text, whichever you wish to move, and release the mouse button. Move the mouse to reposition. Left click again to place it. 10. Click Close to exit the dialog. Note: You can copy and paste datum target annotations on the same sheet or paste them on another sheet in the same drawing file. To copy the annotation: click on it to select it (press and hold the Shift key to select multiple annotations). Then, either right click and choose Copy; or, from the Edit menu, select Copy. To paste the annotation: you can choose Paste from the Edit menu, or you can move your mouse to the location you want to paste the annotation and press CTRL + V on your keyboard. 21

26 The datum target symbol can be repositioned by clicking the text and dragging. This will change the length of the leader, as well as reposition the datum target symbol. Datum targets can also be moved to another location by clicking the arrow, as opposed to the text Feature Control Frames The geometric tolerance annotations let you specify a reference frame that contains all the geometric tolerance information for a selected surface or feature. The annotations support both the ANSI Y14.5 M-1982 and the 1994 standards. You also include datum references if the geometric tolerance is related to a datum. You reference primary, secondary, and tertiary datum reference frames with the following material conditions for each geometric tolerance: (M) MMC-maximum material condition (L) LMC-least material condition (S) RFS-regardless of feature size (F) Free State-not limited by state position. 22

27 To create a feature control frame: 1. In any type of workspace, from the Insert menu select Annotation > Feature Control Frame. In a drawing workspace, select the Feature Control Frame tool from the Detailing toolbar. The Feature Control Frame dialog appears. 2. If the geometric tolerance is related to a datum, specify as many as three datum references that form the Datum Reference Frame. For the primary, secondary, and tertiary datums: Click the Datum reference letter. (The reference letters were created when you inserted the Datum annotations.) Click the MC arrow for the datum, and select the material condition for that datum. 3. Click the Symbol arrow, and select one or more of the displayed tolerance symbols. The geometric tolerance symbols indicate controls for form, profile, orientation, location, and runout. 4. Specify the allowed Tolerance values. 5. Select the Diametrical Tolerance symbol if the tolerance is associated with a diameter zone. 6. Select a material condition from the MC pull-down menu for each tolerance value. 7. Repeat steps 2-6 on the Feature Relative tab if you want to specify a stacked feature control frame. This allows you to see a different symbol for each row. If you want a composite tolerance instead (one symbol shared across rows), check the Composite Tolerance checkbox. 23

28 8. Select the Projected Tolerance option if required and specify the Height of the projected tolerance zone. 9. Select the Standard that you want to use for the tolerance symbol. Alibre Design supports ANSI Y14.5 M-1982 and The preview shows the symbol for the selected standard. 10. Select the Between Points option to call out a tolerance between two points. Enter labels for the two points. 11. Select the Show option to include a leader, the Bent option if desired, and select an Arrow type. 12. Select Smart Anchor if necessary. 13. Move the mouse in the work area. A preview of the annotation appears attached to the mouse pointer. Left click once to place the leader line. Left click again to place the annotation. The text appears in light blue. 14. Click Apply to accept the annotation placement (or you can double-click). The dialog remains open so you can continue to place additional annotations. Before choosing Apply, you can reposition the annotation while it is light blue in color. To do this, left click on the leader line or the text, whichever you wish to move, and release the mouse button. Move the mouse to reposition. Left click again to place it. 15. Click Close to exit the dialog. Note: You can copy and paste feature control frame annotations on the same sheet or paste them on another sheet in the same drawing file. To copy the annotation: click on it to select it (press and hold the Shift key to select multiple annotations). Then, either right click and choose Copy; or, from the Edit menu, select Copy. To paste the annotation: you can choose Paste from the Edit menu, or you can move your mouse to the location you want to paste the annotation and press CTRL + V on your keyboard Surface Finish Symbol In drawing, part, or assembly workspaces you can specify the surface texture of a face by using a Surface Finish Symbol. In a part or assembly, you can attach annotations to solids. In a drawing, you can attach annotations to any view, or to the projected edge of a model. 24

29 To create a surface finish symbol: 1. In any type of workspace, from the Insert menu select Annotation > Surface Finish. In a drawing workspace, select the Surface Finish tool from the Detailing toolbar. The Surface Finish dialog appears. 2. From the Symbol pull-down menu, select the machining method for the surface finish. 3. From the Lay Direction pull-down menu, select the direction of the surface pattern. 4. In the Roughness area: Specify a value for the Maximum allowable height deviation from the surface mean plane. Specify a value for the Minimum allowable height deviation. Specify a value for the average Spacing of roughness peaks. Specify a value for the roughness Sampling length. 5. Select the symbol Standard that you want to use. Alibre Design supports ANSI Y14.16, ISO 1302, and JIS Symbols. 6. In Material Removal, specify the value for the amount of stock to be removed by the machining method that you selected. 7. In the Waviness area: Type a value for the Waviness (peak-to-valley height) of the waves. Type a value for the Spacing between adjacent peaks. 8. If you want to specify the Production Method to be used for the surface finish, type it in the box provided. 9. If you want to include a leader: Select Show. Select Bent if you want the line to have a short horizontal segment near the annotation. Click the Arrow down arrow, and select a style. 10. Move the mouse in the work area. A preview of the annotation appears attached to the mouse pointer. Left click once to place the leader line. Left click again to place the annotation. The text appears in light blue. 11. Use the Rotation Angle to change the angle at which the symbol is displayed. 25

30 12. Check the Flip Text box if you desire to flip the text 180. Note: The Flip Text box will automatically become checked if the rotation angle goes above 90. However, you can uncheck the box if you do not want the text flipped. 13. Click Apply to accept the annotation placement (or you can double-click). The dialog remains open so you can continue to place additional annotations. Before choosing Apply, you can reposition the annotation while it is light blue in color. To do this, left click on the leader line or the text, whichever you wish to move, and release the mouse button. Move the mouse to reposition. Left click again to place it. 14. Click Close to exit the dialog. Note: You can copy and paste surface finish annotations on the same sheet or paste them on another sheet in the same drawing file. To copy the annotation: click on it to select it (press and hold the Shift key to select multiple annotations). Then, either right click and choose Copy; or, from the Edit menu, select Copy. To paste the annotation: you can choose Paste from the Edit menu, or you can move your mouse to the location you want to paste the annotation and press CTRL + V on your keyboard Weld Symbol To create a weld symbol: 1. In any type of workspace, from the Insert menu select Annotation > Weld. In a drawing workspace, select the Weld tool from the Detailing toolbar. The Weld dialog appears. 2. Click the Far or Near tab, depending on where you want the annotation placed in relation to the design. 3. From the Finishing method pull-down menu, select the method that you want to specify. 4. From the Contour pull-down menu, select the shape that you want for the weld surface. 5. Specify a Groove angle value in degrees. 26

31 6. Specify a Root opening value. 7. In the Weld symbol area, select the weld symbol from the pull-down menu. You can also type text into the boxes on both sides of the weld symbol. 8. In the Joint with spacer area, select the spacer type from the pull-down menu. 9. Select the applicable weld placement options: All around Field or site weld Display pointing down (enabled if you select Field or site weld) Stagger weld (enabled if you select a fillet for both the Near and Far tabs) 10. In the Specification process area, type any additional instructions to be included with the weld symbol. 11. If you are specifying both a Near and a Far weld, click the other tab, and repeat the steps for the other weld. 12. If you want to include a leader: Select Show. Select Bent if you want the line to have a short horizontal segment near the annotation. 13. In Arrow, select an arrow style. 14. Move the mouse in the work area. A preview of the annotation appears attached to the mouse pointer. Left click once to place the leader line. Left click again to place the annotation. The text appears in light blue. 15. Click Apply to accept the annotation placement (or you can double-click). The dialog remains open so you can continue to place additional annotations. Before choosing Apply, you can reposition the annotation while it is light blue in color. To do this, left click on the leader line or the text, whichever you wish to move, and release the mouse button. Move the mouse to reposition. Left click again to place it. 16. Click Close to exit the dialog. Note: You can copy and paste weld annotations on the same sheet or paste them on another sheet in the same drawing file. 27

32 To copy the annotation: click on it to select it (press and hold the Shift key to select multiple annotations). Then, either right click and choose Copy; or, from the Edit menu, select Copy. To paste the annotation: you can choose Paste from the Edit menu, or you can move your mouse to the location you want to paste the annotation and press CTRL + V on your keyboard Editing and Deleting Annotations You can edit or delete an annotation anytime after it has been created and placed. To edit or delete an annotation: 1. Select the Select tool from the View toolbar. 2. Move the cursor over the annotation. The annotation is highlighted and the cursor includes the symbol icon when it is over the annotation that can be edited or deleted. 3. Right-click the annotation and select Edit or Delete from the pop-up menu. In the Edit case, the Annotation dialog appears. 4. Make the necessary changes to the annotation properties. To move an annotation: 1. In the workspace, click an annotation, then without releasing the button, drag the annotation. You can align an annotation with other annotations when you drag it. To turn this option on and off, from the Tools menu, select Options. On the General tab, check (to turn on) or uncheck (to turn off) Align annotations when dragging. When this option is checked on, you can press and hold the CTRL key to override it. Or, 1. Right-click the annotation you would like to change and select Edit. The original dialog appears. 2. In the workspace, click where you want to move the annotation. 28

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